Skip to main content
P
ptc-52468401-Visitor
1-Visitor
October 7, 2014
Solved

Fix displacement in only +ve direction for non-linear analysis?

  • October 7, 2014
  • 2 replies
  • 17742 views

Hello,

I am performing non-linear static analysis and have the following 2 questions:

1. I want to constrain a surface such that it is not allowed to move in the +Z direction but free to move in the -Z direction.

Z is normal to the surface.

2. Secondly I want to know whether the displacement can be made a function of time similar to loads?

Best answer by sdensberger

I'm a little confused on what your analysis setup is suppose to be for the assembly level or what the goals of the analysis are (stress, displacement, etc.). Could you put something together describing the real-world problem you're trying to simulate and what you want to capture.

For your part level analysis, part of the reason why your analysis took so long to run is that you're having numerical stability issues. If you look in the .PAS file, you'll see several pseudo time steps are taking 100-150 iterative steps to convergence on an acceptable residual nor level, and on a couple different occasions your stiffness matrix becomes singular. If you look at the first pass results, you'll see that the outer most tip of the flange displaces more that its radius; this means that you applied load is now going to be a (mostly) shear load on the surface. This in combination with the very large displacements you're having is part of the reason why the analysis is taking so long to run.

Now, if you want to try to approximate a contact surface between the inner curved surface of the rubber part, then you could create a cylindrical coordinate system and constrain the surface in the radial direction (but remember, the surface will not be able to move in the + or - R direction). Looking at the stress-strain curve for your hyperelastic material models makes me think that this assumption isn't too bad. From a strain of 0 to 5 your stress increases by about 30 MPa, giving a linearized Young's Modulus of about 6 MPa; after that, the next linearized Young's Modulus would be about 50 MPa. Your base material has a Young's Modulus of 7 GPa, so we have about 2-3 orders of magnitude greater stiffness on the base. You can see how this helps reduce the displacements, but you will have the flange deformed to a vertical position. At this position do you really expect to have a 10 N load vertically down (which, for the deformed shape, would be something like a friction load).

Displacement.png

Yeoh.png

2 replies

S
sdensberger2-Explorer
2-Explorer
October 7, 2014

I want to constrain a surface such that it is not allowed to move in the +Z direction but free to move in the -Z direction.

You're not going to be able to do this directly. What you're describing is a contact conditions (stiffness is unit-vector dependent); a constraint is specifying the displacements (knowns and unknows) for points/edges/surfaces on the element(s) and it's something that you won't be able to "turn-off".

Secondly I want to know whether the displacement can be made a function of time similar to loads?

You can make enforced displacements a function of pseudo-time; this is done by clicking the "f(x)" button under "Time Dependent" in the constraint box (you'll see "Ramp" next to "f(x)" by default). Keep in mind that the y-value of your function/table defines the scalar value of the enforced displacement. If you have an enforced displacement value of 3e-3 in, then when the time-dependent function/table has a y-value of 1, the value of the enforced displacement will be 3e-3 in (likewise, a y-value of 2 will be an enforced displacement value of 6e-3 in).

    P
    ptc-52468401-VisitorAuthor
    1-Visitor
    October 16, 2014

    Hi Shaun,

    I appologise for the delay as I was out of office until today.

    1. I dont think this constraint will define the displacement of the nodes, it will only limit the displacement in one direction. All other DOFs are free. Additionally, the planar constraint is quite apposite for this task. But I am unable to comprehend why it is allowed only for SDA and not for LDA.

    2. What you say is correct, but that is not what I require. I want to fix some of the DOFs of some nodes for a specified time interval and for the remaining time interval these DOFs are free and unconstrained. I tried to make the displacement constraint a function of time, but it has no effect, which seems logical considering displacement constraint makes displacement zero and plotting a graph of displacement vs time is irrelevant as 0 X anything(value from graph) = 0. So eventually the fix displacement will apply for the entire time interval. Thus Simulate does not allow such situation to be simulated, however it is a perfectly valid situation and could be supported in future releases. What do you say?

    S
    sdensberger2-Explorer
    2-Explorer
    October 17, 2014

    1. I dont think this constraint will define the displacement of the nodes, it will only limit the displacement in one direction. All other DOFs are free. Additionally, the planar constraint is quite apposite for this task. But I am unable to comprehend why it is allowed only for SDA and not for LDA.

    A constraint is, by definition, a prescribed nodal displacement. All static structural problems involve solving:

    {f} = [k]{d}

    where {f} defines the forces acting on the system, [k] defines the stiffness matrix of the system, and {d} defines the nodal displacements. Your constraints define your displacement vector {d}; i.e. a "fixed" constraint on a surface defines all nodal displacements (Tx, Ty, Tz, and Rx, Ry, Rz if the element type has rotational DOF) on that surface to be 0. Nodes that have no constraints applied to them are unknowns that need to be solved for. You need to also keep in mind that there are only 6 DOF total (translations in x, y, and z, and rotations in x, y, and z), so there is no way to prevent a node from moving in the -x direction while still allowing it to move in the +x direction. That type of requirement is typically handled via contact, not with a constraint. If you want to prevent a surface from moving in (for example) the -x direction but allowing it to move in the +x direction, you'll need to either create a wall and define a contact set between it and the other part, or use non-linear springs (this may or may not work or be realistic depending on what you're modeling and what you need from a results standpoint).

    2. What you say is correct, but that is not what I require. I want to fix some of the DOFs of some nodes for a specified time interval and for the remaining time interval these DOFs are free and unconstrained. I tried to make the displacement constraint a function of time, but it has no effect, which seems logical considering displacement constraint makes displacement zero and plotting a graph of displacement vs time is irrelevant as 0 X anything(value from graph) = 0. So eventually the fix displacement will apply for the entire time interval. Thus Simulate does not allow such situation to be simulated, however it is a perfectly valid situation and could be supported in future releases. What do you say?

    You're correct: Simulate doesn't allow the user to "turn-off" a constraint during a simulation. While it is a perfectly valid simulation, there might be a technical reason why Simulate doesn't have this feature (or maybe it's not high on PTC's list of Things-To-Do). That being said, there are potential work-around's that may or may not work for your model (I'd need to understand your model to know one way or the other) that involve time-dependent loads and springs.

    G
    gkoch1-Visitor
    1-Visitor
    October 13, 2014

    Hello Sumit,

    did the hints from Steven and Shaun help you?

    Gunter

    P
    ptc-52468401-VisitorAuthor
    1-Visitor
    October 16, 2014

    Hello Gunter,

    As mentioned previously I was out of office until today and I appologise for the delay in reply.

    I am not yet satisfied with the suggestions and am looking forward to further refinement.

    P
    ptc-52468401-VisitorAuthor
    1-Visitor
    October 19, 2014

    Hello Steven,

    I have uploaded a simplified model similar to my requirement.

    http://communities.ptc.com/servlet/JiveServlet/downloadBody/6419-102-1-9748/17.10.2014.zip

    The contact analysis in my case is taking tremendous time, so I wanted to run an equivalent simulation only on the rubber part.

    Let me know which set of constraints could approximately give similar results as the contact analysis?

    Terms & ConditionsAccessibility statement